fvMeshDistributors: New library for mesh redistribution and load-balancing

Basic support is now provided for dynamic mesh redistribution, particularly for
load-balancing.  The mesh distributor is selected in the optional 'distributor'
entry in dynamicMeshDict, for example in the
multiphase/interFoam/RAS/floatingObject tutorial case when run in parallel using
the new Allrun-parallel script

distributor
{
    type            decomposer;

    libs            ("libfvMeshDistributors.so");

    redistributionInterval  10;
}

in which the 'decomposer' form of redistribution is selected to call the mesh
decomposition method specified in decomposeParDict to re-decompose the mesh for
redistribution.  The redistributionInterval entry specifies how frequently mesh
redistribution takes place, in the above every 10th time-step.  An optional
maxImbalance entry is also provided to control redistribution based on the cell
distribution imbalance:

Class
    Foam::fvMeshDistributor::decomposer

Description
    Dynamic mesh redistribution using the decomposer

Usage
    Example of single field based refinement in all cells:
    \verbatim
    distributor
    {
        type            decomposer;

        libs            ("libfvMeshDistributors.so");

        // How often to redistribute
        redistributionInterval  10;

        // Maximum fractional cell distribution imbalance
        // before rebalancing
        maxImbalance    0.1;
    }
    \endverbatim

Currently mesh refinement/unrefinement and motion with redistribution is
supported but many aspects of OpenFOAM are not yet and will require further
development, in particular fvModels and Lagrangian.

Also only the geometry-based simple and hierarchical decomposition method are
well behaved for redistribution, scotch and ptScotch cause dramatic changes in
mesh distribution with a corresponding heavy communications overhead limiting
their usefulness or at least the frequency with which they should be called to
redistribute the mesh.

tutorials/multiphase/interFoam/RAS/floatingObject/system/blockMeshDict

@@ -46,6 +46,7 @@ boundary
             (0 4 7 3)
         );
     }
+
     atmosphere
     {
         type patch;
@@ -54,11 +55,18 @@ boundary
             (4 5 6 7)
         );
     }
+
     floatingObject
     {
         type wall;
         faces ();
     }
+
+    internal
+    {
+        type internal;
+        faces ();
+    }
 );
 
 

tutorials/multiphase/interFoam/RAS/floatingObject/system/decomposeParDict

@@ -16,7 +16,7 @@ FoamFile
 
 numberOfSubdomains 8;
 
-method          scotch;
+method          hierarchical;
 
 simpleCoeffs
 {
@@ -25,7 +25,7 @@ simpleCoeffs
 
 hierarchicalCoeffs
 {
-    n               (2 2 1);
+    n               (2 2 2);
     order           xyz;
 }